OP amp simulation problems
3704 10
lu.nemec 6 years ago
Hello, I have problem with running spice simulation on my circuit: https://easyeda.com/editor#id=0pjPJDVP7 Error: unknown subckt: xu4 d6_a xu4_2 c8_1 tl082 I have looked for other answers here on the forum, but none helped. I tried and found spice file for the TL082 (http://www.ti.com/product/tl082) but when I added it to the schematic, the spice instead said out of memory ... Any ideas? Thank you, Lukas
Comments
example 6 years ago
Hi Lukas, * Let me try to explain the problem. You have placed two instances of the EasyEDA `parameterised 3 pin opamp`. When you place this in a schematic it calls up it's own spice model called `opamp3pEE`. This model has a number of parameters - based on values available from most device datasheets - that the user can adjust via the right hand Properties Panel to tailor the model to a wide range of devices. However the `parameterised 3 pin opamp` is not suitable for use with either any other EasyEDA or 3rd party opamp models. Hence you cannot rename the symbol to try to call up any other model. It is worth noting that there is also an EasyEDA `parameterised 5 pin opamp` uses the `opamp5pEE` model which has supply pins and some additional parameters but is otherwise used in the same way as the `parameterised 3 pin opamp` and also is not suitable for use with either any other EasyEDA or 3rd party opamp models. * If you want to include a TL082 device in a simulation schematic then you have a couple of choices. First though, you must appreciate that even if you have a model for a TL082 or a TL084, this will almost certainly be a model for only a single opamp and will be configured for use with a 5 pin opamp symbol and not a dual or quad opamp symbol. 1. Use the EasyEDA `5pin Operational Amplifier` >1. Place a `5pin Operational Amplifier` symbol; >2. Edit the name to `TL081EE`; This calls up the `TL081EE` model. This is a version of the `opamp5pEE` with fixed parameters tailored for the TL081. 2. Use the EasyEDA `5pin Operational Amplifier` >1. Obtain a 3rd party spice model for the TL082 (Or the TL081 or TL084: they are almost identical); >2. Paste it into your schematic; >3. Select the text and do: >> **Properties > text type > spice** >4. Place a `5pin Operational Amplifier` symbol; >5. Edit the name to be identical to that of your spice model; The symbol then calls up the model you have pasted into the schematic. For more information, please see: >`Attaching a .subckt to a symbol 01` and; >`Attaching a .subckt to a symbol 02` in: ><https://easyeda.com/example/Spice_tutorials_02-YxrJ1Vd7p> This recent forum post may also be helpful: ><https://easyeda.com/forum/topic/Dual_op_amp_spice_simulation-9HBvN4Ygy> Does that help? Questions? Just ask.
Reply
example 6 years ago
Lukas, I should also have said that you can use the `3 pin parameterised opamp` symbol but you have to keep the name of `opamp3pEE` and you have to edit the parameters to those of the TL082. Similarly you can use the `5 pin parameterised opamp` but you have to keep the name of `opamp5pEE` and you have to edit the parameters to those of the TL082. :)
Reply
lu.nemec 6 years ago
Hello, thank you for your response, the schematic now simulates. I have another question, how can I find out the precise spice model for given IC? Say I want to change TL081 for NE5532, what model name would I choose? Is there some catalog of parts that have spice model? Thank you, Lukas
Reply
andyfierman 6 years ago
Hi Lukas, Glad that helped you out. :) A spice model search tool is in development. In the meanwhile, the easiest way to work around this is to find and paste the relevant spice model into the schematic, change the pasted text type to ` spice` and edit the symbol name to the exact same as the spice model name as described above. If you need help on finding and getting models working please post back. :)
Reply
DrSavitaGaur 8 months ago
Good morning Im not able to use TL064CDT ic in easyEDA while simulating circtuit also TL064C individual 3pin/5 pin ICs also not able to use . as it not giving the normal buffer function kindly help and suggest solution
Reply
andyfierman 8 months ago
Please read the Simulation Tutorial.
Reply
DrSavitaGaur 7 months ago
@andyfierman hi Simulation tutorial from where How to make spice model of TL064 in easyEDA What is .param, and used for adding spice model \-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\- Vacoustic_pressure = Acoustic pressure signal model. 1Pa = 0dBA => 1Vrms Set to -35dB in this simulation.
Reply
andyfierman 7 months ago
@DrSavitaGaur, * You will find a link to the Simulation Tutorial by reading and following the linked documents in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) * You do not need to "... make spice model of TL064 in easyEDA". It is already in the library as explained in my reply to you in: [https://easyeda\.com/forum/topic/Include\_spice\_model\_from\_internet\-NnhVdvpHY](https://easyeda.com/forum/topic/Include_spice_model_from_internet-NnhVdvpHY) * The .param spice statement is not "used for adding spice model". The use of .param described in the Simulation Tutorial. * The relevance of this extract : \-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\-\- Vacoustic_pressure = Acoustic pressure signal model. 1Pa = 0dBA => 1Vrms Set to -35dB in this simulation. from my electret microphone model and simulations in: [https://easyeda\.com/andyfierman/Projects\_for\_beginners\-tqkewO60i](https://easyeda.com/andyfierman/Projects_for_beginners-tqkewO60i) can be understood by reading the Simulation Tutorial as explained above. <br> <br>
Reply
Markus_ee 6 months ago
Hi! If you also want to try circuits around opams in a real world scenarios, then I suggest to build an experimental prototyping board to tinker with various implementaions around an opamp. Sometimes this approach works better than just a simulation. You could try to build one of my projects that is just perfect for this occasion: [https://easyeda.com/markus_jidoka/OpAmp-Tinker-Board-v2.0](https://easyeda.com/markus_jidoka/OpAmp-Tinker-Board-v2.0)<br> <br> I got an idea for this from the Youtube channel known as "learnelectronics" Regards, Markus Virtanen HW / Electronics Designer
Reply
andyfierman 6 months ago
Not to detract in any way from the suggestion by @Markus_ee, but it is worth noting that the EasyEDA in-house opamp - and many other device - models created for EasyEDA by signality.co.uk are specially designed to behave as closely to real world devices as possible. This is not always true of manufacturer supplied device models. For example the EasyEDA in-house model **opamp5pee** available in the EELib and used as - via a simple set of user editable datasheet parameters - the core of the TL071EE, TL081EE, LF355EE, LF356EE and other devices in the Spice Symbol library models: * quiescent and load dependent supply currents; * inputs common mode and differential input limits;  * input offset voltage is normally zero but can be adjusted if required;  * inputs bias currents (bias current offset can be adjusted if required);  * input capacitances;  * input resistances;  * output swing vs load;  * output short circuit behaviour including supply current drains;  * device shutdown on minimum supply rail limits;  * exceeding absolute maximum supply rail limits or reverse supply voltage causes skyrocketing supply currents to indicate catastrophic device failure;  * input or output over-rail events (inputs or outputs exceeding the rails) causes skyrocketing pin currents to indicate catastrophic device failure;  * slew rate (although not slew rate asymmetry that some devices exhibit);  * gain bandwidth;  * and on devices such as the TL07n and TL08n, they correctly model output inversion when the inputs exceed the specified input common mode limits. Some of these features are demonstrated here: [https://easyeda\.com/andyfierman/The\_EasyEDA\_5\_pin\_parameterised\_opamp\_model\-7HBTNtKEW](https://easyeda.com/andyfierman/The_EasyEDA_5_pin_parameterised_opamp_model-7HBTNtKEW)<br> <br> Similar realistic behaviours and parameters are modelled across the whole range of in-house EasyEDA models from signality.co.uk including several of the comparators based on the compOC6pee model (again thanks to a simple set of editable datasheet parameters) and the whole of the 74HC digital spice symbol library which accurately models supply dependent propagation delays and rise and fall time behaviour. [https://easyeda\.com/andyfierman/Inverting\_comparator\_with\_hysteresis\-87a982dc29b24c1cb835e939a0659d70](https://easyeda.com/andyfierman/Inverting_comparator_with_hysteresis-87a982dc29b24c1cb835e939a0659d70)
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版,使用建立访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程,下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow
We use cookies to offer you a better experience. Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site, you consent to the use of our cookies.